I have a part on my unicycle (well two) where there's a very tight slip fit on a 3/4" 48 spline interface. I'd like to make one of these (manual machines, sadly no CNC), and I'm wondering what kind of tolerances you would choose on these things. Yes, I understand that the size and shape of the splines matters, but I don't have the tools to measure this. I would figure they are at most 0.075" tall. The material is 4130 cro-mo for both parts, although the axle is occasionally done in titanium.

Furthermore, what would you use to make this? I was thinking a dividing head on a VERY beefy horizontal mill (I have a friend who will let me use his gigantic KT). Get a cutter with the shape of the splines, and do a single, full depth pass. Use the removal of the cutter as a finish pass, using the flex of the mill to allow it a bit more meat to smooth out. Once I have the axle made, grind a HSS cutter to fit with these splines, and put it in a small boring bar on a shaper.

The issue I have is that there's only one shot on the shaping of the internal splines. I can't imagine being able to take down and remount the part in order to test the interface.

Sorry if this is an elementary question for some of y'all. It seems rather difficult for me, mostly because I'm not even sure how exactly to tolerance the splines.

I would make a broach fort the internal splines, but from what I understand, splines of that size require gigantic broaches. Also, I don't have an arbor press that could drive a broach of the size I figure I would need. Is it possible to make a single tooth broach that runs in an indexing collar? It would index off one initial spline that is cut on the shaper. That way if the splines are slightly too tight, I can just shim the broach and cut a bit more off?

For this type work, not having CNC isn't really a drawback, especially when making one or two of a part.

With 48 splines on a 3/4 diameter, I'd assume this is a serration type spline as opposed to a square shoulder or an involute form?

The external spline can be cut on a horizontal mill using a dividing head and tailstock support. For a serration spline you might want to design the V angle based on commonly available V type milling cutters. That eliminates having to grind a cutter. If the angle is one where no standard cutter is available, then it would be easier to make a single point cutter and flycut the spline. For the internal spline your best bet is to make a single point tool and "drag broach" it in, one tooth at a time. This can be done with a shaper or it can also be done with the spindle of a mill so long as you have a means of locking it so it cant rotate. In either case, a dividing head or rotary table with indexing plates can be used to index the part. I'd do the external one first, and then make sure my setup on the internal one allows room to check the fit without removing the part from the setup.

Stuff like this can be a bit tedious and time consuming to set up, but to me its the type of work that's really the most enjoyable.

Added: something I've thought about doing but havent tried is to make a hardened form tool that could be pushed thru a hole to form a spline with no metal removal, somewhat like form tapping. I've got an application where i could use this if it works, but havent had time to try it yet. If it does, it would make an internal spline in my part a quick and simple thing. BUT, my part is 6061-T6 and not 4130. Might be worth a try though since you'd already be set up to make the tool while you've got your setup in place for cutting the external spline.

You can take a .075 DOC even with a small horizontal with the type cutter you'll be using. When you put a milling cutter on a supported arbor, the resulting stiffness is like nothing you've ever seen before if your prior experience is with vertical knee mills.

I've got a 12" Brown & Sharpe dividing head, and one of the little 6" no-name chinese or taiwanese ones, and for things like spline cutting, the little one has never failed me yet as far as indexing accuracy is concerned. I think you'll have no problems on that account for what you're trying to do.

For a serration type spline, you can measure the depth by placing thread wires in the V's on opposite sides of the part and measuring across the wires. The simplest thing to do is determine in advance what your measurement across the selected wires will be when the splines are cut to the proper depth, and to also calculate the relationship between differences in measurements across the wires and how that relates to how much additional downfeed you need to get to the right depth. When you're making a part using a dividing head, the work needs your full attention lest you forget where you are and scrap the part. Any involved calculations that can be done beforehand shouldn't take place in the middle of making the part.

While its definitely possible to cut the spline on a taper, I really doubt its necessary, and there's no question it will complicate your job by an order of magnitude. If you cut the parts to a close fit initially, you'd most likely be too old to pedal before you get enough wear to result in a sloppy fit

If your spline does have the same profile as a standard V thread, then you can definitely buy a standard V type milling cutter to cut the external spline. Calculate the feedrate based on cutter size and number of teeth, and use that feedrate or something close to it. The large number of teeth on milling cutters tends to make anyone who's used to 2 and 4 flute endmills think the cutter is being fed too fast when its really at the proper feed. Underfeeding the cutter will kill it quicker than most anything else, particularly on a tough material like 4130.

FWIW, the serrated type splines that I've cut seemed to be done with a 90 degree corner, such as the corner of an endmill. This is done without too much fuss, just using a vertical mill, and dividing head of course, and working at the 1:30 o'clock position. Or, if you want to work on top of the part with depth adjustments made in only the Z axis, tilt the head 45 degrees and have at it.

I don't know about getting a precise fit on the internal splines other than making a guage spline in the same setup as your male spline. A tight slip fit is almost a zero tolerance, so if you don't want to pound the thing together, a bit loose would be better, and a bit of loctite to fill up the gap, is what I would recommend.

Another option might be to cast the internal spline around the axle with an epoxy metal. Or, how about a plastic spline insert...something that will displace a little bit with a press fit?

There is something you can try I have had success in the past. Make up your male parts using the fly cutter or some other method but make one shaft out of tool steel but only have about 5mm to 10mm of spline on the end, undercut the back. round off all the sharp edges(front face) and polish as best you can. Now broach your female spline almost to size then using you tool steel broach (hardened of course) and push it through using quite a lot of cutting or soluble oil by doing this a number of times you can end up with a very neat fit and a very good finish in the internal bore. Best if you have the use of a fly or hand broach press to keep things straight. Do not try to "swage" out to much or it will pick up and that will be the end. This process is or was used in rifle barrels using ball bearings for sizing.
regards
Andrew S

Take a close look at those splines. I'm almost ready to bet they are tapered about 3/4" per foot.

Splines are checked for compliance with standards by miking them over pins laid in the tooth space of the male part. There's some standard shop mathematice used to convert the over-pin measurement to a pitch diameter. Machinery's handbook or the Van Keuren book will tell you how.

Forrest is probably right, there is more to the geometry than meets the eye. Be sure you check it out for the overwire dimensions, minor diameter, major diameter and pressure angle.

We form splines with shaping, broaching, hob milling and specialized endmill tools. Your method on the indexing head will work fine for 1 or 2 pieces as long as your cutting tools are correct.

With a diameter of 3/4" and 48 teeth, I would be surprised if you truly have a 45° pressure angle. 30 or 37.5 would be more typical based on my limited experience. This is due to the math involved in designing the spline and getting the correct profile with this number of teeth on this diameter.

Thank's for all this help. I figured making one of these things was involved, now I understand how much.

The splines on the original parts aren't tapered, I have checked this. The reason they aren't is that the cranks (which are the parts with the feamle splines) have to be able to be tightened to squeeze the bearings on the hub together.

Alas, these splines do wear, a surprising amount. I have two hubs with these interfaces, and when i got them I had to pull the cranks on using a screw, and remove them with a bearing puller. At that time, even without the retaining bolts, the crank wouldn't move in any direction. Now, on 5" cranks, there is about 0.01" of radial play as measured from the end of the crank.

I have snapped cotter pinned axles, bent square taper press fit cranks, and twisted an axle on one of the hubs I've described. No, I don't understand how a 150lb person twisted a 3/4" piece of tempered 4130 any better than you.

As for locktite, I have used permanent locktite to fill gaps in these splines before, and after 2 rides there was play in the crank, and when I removed it, plenty of locktite dust in there (granted, removing the crank may have been what turned the locktite to dust, however it wasn't very difficult to remove the thing).

Thanks for the information. I at least now understand how to meausre these splines, and now know that the spec I've been giving for the splines is essentially useless. I *should* spec it by pitch diameter and number of splines, correct? I think I'll do these arbitrarily, as in I won't follow the initial part I'm copying to the letter. Rather, I'll just pick a spline depth and take note of it and use it.

As for using an endmill, that seems interesting. I might try that with a hunk of aluminum just to see how it turns out.

These sound like the shaft treatment given to motorcycle trans shifter actuators. Aren't these just a glorified knurl? There is no metal removed merely the metal is flowed till a desired OD is acheived, knurl teeth are matched to the desired shaft diameter and thus meshes. Certainly, the manufactures of these shafts are not indexing 48 times! Electric motor shafts have a similar knurl cold rolled into them before the rotor is cast. As I recall this is done with linear knurls , much like gear racks.

Yes, that's known as spline or thread rolling. I hear many higher quality and strength screws get rolled, aswell. These splines aren't rolled, however. I can tell because the splines have a taper at their ends that would fit a horizontal milling cutter perfectly. If they rolled the splines the taper would likely be linear. either way, I don't have the topoling or capability to make a spline rolling machine, which is why I figured a mill and a shaper would be better.

The knurls used for rolling splines DO look like gear racks, however the teeth of them aren't uniform along their entire length. At the center they at barely nubs, while near the edges of the "rack" they are full size. At least this is what I understand from the research I've done on the topic.

Wow, thanks. It surprises me that this standard of spline is from the 1st half of the century, being as the company, Profile Racing, isn't nearly that old. It is possible, however unlikely that they came up with their own standard, aswell...

I have a hard time believing that permanent loctite would be 'eaten out' by any process except a fire.

But there should be an explanation if you do see failure of a loctited joint, and I would be guessing that the parts may not have been clean, but more likely, that the loctite was not properly cured before it was put into service. I like to use a gentle heat of about 150°F on a loctite joint to hasten the cure rate.

In this severe unicycle service , I would make every attempt to make a good mechanical interference fit with the spline and still loctite it afterwards, because there are so many ways that a tight fitting spline can drag and seem tight, without the flanks of the teeth actually fitting tight against one another.

Halcohead,
You're welcome.
Not too suprising, many of the old standards, became just that , a standard, and although they have been superceded they continue to hang on. The ANSI standard for involute splines has been upgraded providing for a range of fits, yet still the old ASA B5.15-1950 kept croping up into the 1990's. My SAE book is the 1962 issue.
Les H.

Posting Permissions

ADVERTISEMENTS

ABOUT Practical Machinist

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.